Frequently Asked Forum Questions

I put together a list of questions that seem to get asked fairly often, along with their answers, so here it is (they're in no particular order). Hopefully-the Forum members -will find it helpful. I will edit this periodically as the software evolves, and I've stopped here with 25 topics. More can be found at FAQ - Part 2.

2018-01-16 edit: I'm happy to report that as of today there is a blog section of the forum dedicated to FAQs. Please see it here: FAQs (Frequently Asked Questions). Most of these topics are covered there. Because this new section will be much easier to navigate I will no longer be editing or adding to these two Discussions, but I will leave them in place since they've been linked to from so many other Discussions.

These questions and answers are related to actually working with SolidWorks. If you have questions about using the Forum please see Forum Posting by Deepak Gupta. (Even if you don't have questions about using the Forum you might learn something.)

To start off, if you have some unexpected behavior, which you have no explanation for, re-boot your computer. Don't just shut SolidWorks down and re-open it, re-start your computer. That will often fix problems, especially if it's been running for a while.

Here is a list of brief descriptions to assist in navigating through the questions and answers.

1. Make a sub-assembly flexible

2. Sheet formats and drawing templates

3. Future version error message / backwards compatibility

4. Student version watermark/icon

5. Assembly referencing the wrong Toolbox part

6. Lost orange highlight before selection

7. Poor quality when saving as .pdf

8. Weldment profile sketch not working

9. Annotations wrong color or not showing in drawing

10. Part in assembly won't move

11. Creating realistic threads

12. Linking drawing view balloon to BOM

13. Graphics issues

14. Crop View icon grayed out

15. Showing single bodies of a multi-body part in a drawing view

16. Dimensioning to the edge of a circle or radius instead of center

17. Need a drawing view other than the standard Front, Right, Top, etc.

1. “I have an assembly that is able to move, such as a hinge, or a hydraulic cylinder with a shaft that moves in and out. I inserted it into another assembly and now it won’t move. What happened?”

By default (and no, there isn't any way to change this), sub-assemblies that have some movement are rigid when inserted into another assembly, but they can be made flexible. Find the sub-assembly in the upper-level assembly tree and click on it. Choose the "Make Component Flexible" icon. It should now have the same amount of freedom that it had in it's own file.

I believe this icon was first available with SW 2014. If you're using an earlier version you will need to choose the “Component Properties…” icon instead.

That will take you to the Component Properties dialog box. “Rigid” will be selected by default in the “Solve as” section. Select “Flexible” instead, then “OK”.

By the way, if you have a Limit Mate in your sub-assembly it will probably be broken when you insert it into the main assembly. Delete the Limit Mate from the sub-assembly and apply it in the top level assembly instead. (2016-09-27 Edit: I rarely use Limit Mates, but I have seen reports here on the Forum that this has been much improved with SW2016, so if you're using 2016 or later you might give it a try.)

2. “I made changes to my sheet format and saved it, but when I start a new drawing with a drawing template that uses this sheet format the changes aren’t there. Why?”

The answer to this specific question is in the second paragraph of this reply, but I’m going to give some background first, because understanding the difference between sheet formats and drawing templates confuses many new users. I know it took me a while to get straight. Sheet formats (slddrt files) and drawing templates (.drwdot files) are two distinct different file types. Sheet formats control, among other things, sheet size, sheet orientation (landscape or portrait), and title block notes. Layers are also saved in sheet formats. You can edit a sheet format by clicking on a blank part of the sheet, the sheet tab, etc. and choosing "Edit sheet format" from the drop-down. Right-click again and choose "Edit sheet" to exit the sheet format editing function and return to normal operation. You can save your sheet format by going to File and selecting "Save sheet format" from the drop-down.

You can change to a different sheet format by right-clicking on the sheet tab, the sheet name in the tree, or on a blank part of the sheet, and choosing “Properties…”. That will take you to the Sheet Properties dialog box (screenshot below), where you can set the sheet scale, change or Reload the sheet format, name the sheet, etc. When inserting a new sheet, it will use the same sheet format as the active sheet. (If you don't want it to use the same as the active sheet by default, go to Tools > Options > System Options > Drawings and check the box for “Show sheet format dialog when adding new sheet”.)

If you've saved your sheet format correctly, but none of it shows up on your drawing, make sure that "Display sheet format" is selected in Sheet Properties. It should be selected by default, but you never know.

Drawing templates contain a sheet format (or possibly multiple formats if there are multiple sheets), and an almost unlimited number of settings that are controlled at Tools > Options > Document Properties. Drawing templates are saved by going to “Save as” and selecting "Drawing Template" from the drop-down for file type.

When you start a new drawing using a saved drawing template it will use the sheet format as it existed when the drawing template was saved. The drawing template does not maintain a link to the .slddrt file, so if the sheet format is edited it will not automatically update in drawings. If you want your drawing template to reflect changes to a sheet format you can start a new drawing, go to Sheet Properties, and click on the Reload button to update the active sheet. If you have multiple sheets saved in your drawing template don't forget to do this for each sheet. Then re-save the drawing template.

The information above about new drawings using sheet formats as they existed at the time the drawing template was saved is also true for existing drawings. If you open a drawing that contains a sheet format that has been edited, you will need to Reload the sheet format to update it to the latest saved version. (2016-10-26 edit: Starting with SW2017 you can change the sheet format for multiple sheets with one operation. See here.)

By the way, I strongly recommend saving all custom document templates, sheet formats, weldment profiles, etc. in a separate location (not in the SolidWorks installation folder) so you won't lose them when you upgrade to a new version. If you're a single user save them on your hard drive (and it wouldn't hurt to back them up somewhere else). If you're in a multi-user environment they should probably be saved on a network so other users can access them, and to help maintain uniformity between users. Be sure to point to the proper location for each file type at Tools > Options > System Options > File Locations.

3.“I’m trying to open a file and I’m getting an error message: Cannot open (file name). Future version. Why?” Or“Can I save a file so that it can be opened by an older version of SolidWorks?”

SolidWorks files can't be opened with an earlier version than the one they were last saved with. I know that isn't true for many programs, such as Word, Excel, etc., but SolidWorks is many times more complex than these programs, and features may have been created with functions that weren’t available in earlier versions, and there are probably other reasons. I think Ryan McVay gave one of the best explanations I've seen in the Discussion I link to a few paragraphs down: "Well, because this would require the software to bear the burden of including feature checks, older code, extra code to do the checking and converting, extra Parasolid version exporting, and file restructuring, etc. to exist in the software. Your install DVD just went from 4GB to 10GB- oh crap that doesn’t fit on dvd anymore! And this would only increase every version because you are carrying legacy code and export tools. This is one of the many, but a big reason, why you don’t have backward compatibility across all CAD packages and why users rely on neutral solid exports like STEP and Parasolid- outside of the kernel and 3d definition."

People have been asking for backwards compatibility for years, and maybe someday it will happen, but it hasn’t yet. Document templates are also not backwards compatible. If a template was saved with SW2015 you won't be able to start a new drawing, part, etc. with it using SW2014. Service packs are backwards compatible within the same version. For example, a file saved with SW2014 service pack 5 can be opened with SW2014 service pack 1.

SW models may be saved as several forms of dumb solids, and then opened with earlier versions, but they will lose the features in the tree. According to Jim Wilkinson (and he would know), Parasolid is your best option when doing this. His response at Re: compatibility between versions was "If you do this, make sure to use Parasolid. Parasolid is the native format of SOLIDWORKS so there is no translation when going back. STL is DEFINITELY a bad choice because it only transfers tessellated data which is nearly useless compared to the original b-rep solid/surface data."

Occasionally someone will ask if there's a way to tell which version was used to save a file if you can't open it. Yes, there is. In Windows Explorer, browse to the folder containing the file. Right-click on a blank space at the top, beside the column names, and choose "More..."

Select "SW Last saved with".

That will add a column indicating which SW version last saved the file.

4.“I have files that were created with the Student Version. I now have the commercial version and would like to use these files. Can I get the Student Version icon/watermark removed?”

That can only be done by the people at SolidWorks. They may or may not agree to do so, depending on your situation. Contact your VAR (Value Added Reseller, the company you bought SolidWorks from).

5. “I made some changes to a Toolbox part, and then saved it with a new name in a different folder. I used it in an assembly, saved, and closed, but then when I opened the assembly it’s been replaced by another Toolbox part. What happened?”

This will fix the problem, but you might want to consider removing the Toolbox designation from these parts. Run the sldsetdocprop.exe utility at SolidWorks\Toolbox\data utilities. Set the property state to “No”. Be sure to close any Toolbox parts before running this utility.

6. “When I hover my cursor over a line or edge, it no longer turns orange to preview what I’m about to select.” What happened, and how do I get it back?”

Go to Tools > Options > System Options > Display/Selection and check the box for “Dynamic highlight from graphics view”. If you had this turned on, and it turned itself off, it’s almost certainly your 3d mouse. The 3dconnexion software temporarily turns off dynamic highlighting while the 3d mouse is manipulating a model to prevent multiple edges being highlighted as they move across your cursor. It's supposed to turn it back on when you release the 3d mouse, and it usually does, but not always. It happens to me occasionally, but not as often as it did a couple of years ago. I don't know what triggers it either. It may do it two or three times in a day for me, then not again for weeks or months.

7. “I saved my SolidWorks drawing as a pdf, and the quality is poor. What can I do to fix it?”

I'm editing this answer. Previously I had just said to print to pdf instead of saving as pdf, which often produces better results. That may still be what you need to do, but I recently saw a Discussion here on the forum where a new user was having problems with a company logo disappearing when saving as pdf. He finally realized that the DPI was set to 96. Changing it to a higher value fixed the problem, so check that first, and see if a higher setting will work for you also. If that doesn't work, then print to pdf instead of saving as pdf.

If you can't print to pdf because you don't have the Adobe software, I've seen several people here on the forum recommend Cute PDF, which I understand is a free program that you can download to create PDF's. As a disclaimer, I don't have any personal experience with it, and John Matrishon posted (at Poor PDF Quality - How do I fix it?): "Everyone be aware that CutePDF the free version does not embed the font into the file. This will become a problem if you are using certain viewers to view PDF files, and if the fonts are not compatible. Anytime you are using "print" to pdf, you are not using SOLIDWORKS functions, you are using the software installed locally on your computer. Save AS pdf from inside SOLIDWORKS is your only chance to combat issues related to SOLIDWORKS, so using CutePDF or any other 3rd party printing software may cause you issues. I suggest thoroughly testing all usages. I'm still having to replace PDF files because someone decided to use CutePDF instead, and anyone else with the view reads hieroglyphics where text and dimensions should be."

8. “I created a weldment profile sketch and saved it, but when I try to use it in the Structural Member function it doesn’t work. What’s wrong?”

When saving a sketch as a library feature part (.sldlfp file) to be used in the Structural Member function on the Weldments toolbar, it’s necessary to have the sketch selected (so it’s highlighted in the graphics area and has the blue box around it in the tree) when you go to Save as…sldlfp. That step is commonly over-looked. After saving the file the Sketch icon will have the green "L" on it if it was saved correctly.

If you've saved the profile sketch correctly, check the folder you're pointing to at Tools > Options > System Options > File Locations > weldment profiles. Keep in mind that you need to have the correct number of sub-folder levels in this folder, and this will vary depending on whether or not you're using configurations in your weldment profile sketches. If you aren't using configurations, then your first level of sub-folders will appear in the Standard drop-down (such as ANSI and ISO), the second level will have sub-folders for the profile Types (HSS Square, Angle, Pipe, etc.), and these folders will contain the individual files (left screenshot below). If you are using configurations then the .sldlfp files will be in the Type folder and you'll choose the desired configuration from the Size drop-down (center screenshot below, HSS Square is the file name). I use both, so my .sldlfp files with configurations are in the same folder as the folders containing the .sldlfp files that don't have configurations (right screenshot).

If they appear correct on your monitor, but print incorrectly, check your printer settings. If they're wrong on your monitor, then it could be several things. Check the following:

a. Go to Tools > Options > Document Properties and check to see which Layer is specified for the annotation type. If this is a dimension then check the settings for each specific dimension type (Linear, Ordinate, Diameter, etc.), since those settings will over-ride the general settings for "Dimensions". If it's wrong, change it and save. If those settings are correct proceed to...

b. Exit from the Options menu and check to make sure that your active Layer is set to "per Standard". If a different Layer is active when placing annotations then this Layer's properties will over-ride the settings at Tools > Options > Document Properties. Also, click on the annotation to select it and check which Layer it belongs to. Change it if needed. If this doesn't work go to...

c. If your Layer settings (in Document Properties and your active Layer) are correct, check the settings on your Line Format toolbar. Make sure that the "Color Display Mode" button isn't depressed. Next click on the "Line Color" icon on the Line Format toolbar and make sure that "Default" is checked.

Just to clarify the hierarchy here, Layer settings will over-ride settings at Tools > Options > Document Properties, and Line Format toolbar settings will over-ride Layer and Document Properties settings.

And if you have notes, dimensions, etc. that are visible on your monitor but don't show up when you print your drawing, check your Layer properties. Starting with SW2015 you can set a Layer to not print. In the screenshot below, the layer BLACK is set to not print. Click on the printer icon to change it's status.

10. “One of the components in my assembly won't move, but it doesn't have any mates."

The first component (Part or Sub-assembly) inserted into an Assembly is Fixed by default. It will have (f) in front of the file name in the tree. If you drag another component above it in the tree it will still be fixed. If you want to move it, just right-click on it and choose "Float" from the drop-down. Now you'll be free to left-click and drag it, right-click and rotate it, etc., or position it with Mates.

By the way, if you placed the first component by clicking in the graphics area, which many users do, then it's position will be more or less random. Instead you can select the component to insert and then click on the green checkmark at the top of the Insert Components PropertyManager without clicking in the graphics area. It will then be fixed with it's three primary planes aligned with the Assembly's primary planes. That's what I almost always do with the first component (and sometimes with later components). If I don't do that then I immediately Float it and Mate it where I want. I never just leave a part where it was placed by clicking in the graphics area.

11. “How do I create realistic threads?"

SW 2016 introduced a thread feature (2016 What's New in SOLIDWORKS - Creating a Cut Thread). If you're using an earlier version, see Threading Options. Please keep in mind that while you can create threads, it doesn't necessarily mean you should. Unless you absolutely need them for 3d printing, or for some other reason, I'd recommend not creating them at all. (Even if you are creating a model for 3d printing, I've seen others here recommend cutting the threads after the part is printed for accuracy.) I rarely create threads. They can drastically slow down performance, especially if there are multiple instances in an assembly, and if you try to attach an annotation leader to threads in a drawing you'll have plenty of time for a break before you can get back to work. I often put a note in my drawings that says something like "Threads not shown for clarity". If you need threads just for visual effects, then go ahead and make them, but if you're using multiple instances of the Part in an Assembly I'd strongly suggest creating a configuration with the thread feature suppressed, and use this configuration in the Assembly.

12. “I have a drawing with a Bill of Materials, but when I try to attach a balloon to a drawing view of a single component the balloon number is always 1. How can I get it to match the BOM?"

Right-click on the drawing view of the component and choose "Properties..." from the drop-down. Check the box for "Link balloon text to specified table", and select the correct table from the drop-down. Beginning with SW2017, after you have linked one drawing view to a BOM, other views will automatically be linked upon insertion (assuming there's only one BOM in the Drawing). (See SW2017 Enhancement That Didn't Make the "What's New" Document.) If you're using an earlier version this will need to be done for each view.

If you have multiple tables in a drawing you might want to name them to avoid confusion when linking drawing views. Left-click on a table in the tree to highlight it, then left-click again (or hit your F2 key) to name tables (this also works for drawing views, features in Parts and Assemblies, configurations, display states, planes, etc.). Naming drawing views and tables may also be helpful if you save drawings as .PDF's, since these names will carry over as Bookmarks.

While I'm on the subject of BOM's, people occasionally ask how to have a BOM by itself on a sheet without the drawing view, such as in complex assemblies where the BOM takes up the whole sheet. Insert the drawing view and insert the BOM, like usual, but after inserting the BOM you can delete the drawing view. After being inserted in the drawing the BOM is linked to the assembly file itself, not the drawing view, and will still update if the assembly is edited, even if the drawing view has been deleted. Because of this behavior, if you have inserted a drawing view of an assembly and a BOM, and then change the drawing view to show a different configuration, the BOM will not automatically update to reflect this configuration. You can go to the BOM's PropertyManager and change which assembly configuration it's referencing. You can also create a BOM and move it to another sheet. Go to your tree, find the BOM, click on it, and drag it to the sheet name of the sheet you want it moved to. You may need to rebuild for the move to take effect.

13. “I have weird graphics issues. What could be causing that?"

Check your graphics card. I am by no stretch of the imagination a hardware expert, but from reading posts here on the forum for years I feel confident in saying that if you have weird graphics issues it's probably your graphics card. The wrong graphics card (or the wrong driver for the right card) can cause an infinite number of strange issues. Some people use unapproved cards with no problem, but you probably aren't lucky enough to be one of those. If you have a company IT person that spec'ed your new machine with a high end gaming card because he/she just assumed it would work well with SolidWorks, you have my sympathies. Get an AMD FirePro or an NVIDIA Quadro (which is what I use) for best results. If you already have one of those, check here to see if you have the correct driver. The newest driver isn't necessarily the one that works best with SolidWorks. You might also run the SolidWorks Diagnostics tool at Start > All Programs > SolidWorks 2015 (or whatever year) > Tools > SolidWorks Rx > Diagnostics to see what that shows.

If you have a GeForce card, and it was working fine but stopped, it's probably because of an automatic driver update. See here.

I've seen a number of Discussions here on the Forum about problems when the Windows icon scale is set to anything other than 100% (especially larger), so if yours is set to something else try switching to 100% and see if that helps.

If you're stuck with a non-approved card, and nothing else works, try selecting "Use software OpenGL" as shown below (Tools > Options > System Options > Performance). I don't have any experience with this, but I understand that it helps sometimes. If it's grayed out so you can't select it then close all SW files and try again.

14. “I placed sketched lines in a drawing to use for a Cropped View, but when I click on one of these lines the Crop View icon is grayed out. What's wrong?"

This drove me half crazy when I was new to SolidWorks. You almost certainly started the sketch outside of the drawing view (so the dotted line box didn't appear around the view). Because of this, the lines don't belong to the drawing view, so you can't use them to crop it. To check this, click on the drawing view and drag it. If the lines didn't move with it, then that's what happened. You can cut and paste these lines, making sure the drawing view is active when pasting, or delete them and start over (again, making sure the drawing view is active when you start sketching). You can double-click on a view to lock it active if needed.

The same is true if you place a sketched line first when creating a Section View. If the sketch doesn't belong to the view then you can't use it.

15. “I have a multi-body part that I need to detail in a drawing, and I would like to show single bodies in some drawing views. How can I do that?"

When you've selected the model to insert in the drawing, go to the "Select Bodies..." button in the drawing view's property manager.

That will take you to the Part file where you can select which body (or combination of bodies) you want to show in the drawing view. You can also use this feature for existing drawing views, not just when you're inserting them. I believe this is the simplest method, and the one I use, but there are a couple of others described below.

Another method is to insert the drawing view, then right-click on an edge of a body you want to hide and choose Show/Hide > Hide Body.

A third option is to save out the bodies as separate Part files by right-clicking on the body and choosing "Insert into New Part..." from the drop-down. A number of people use this method, but I don't think I've ever had a reason or need to.

And the fourth option would be to create multiple Display States in your Part, hiding bodies in each as needed, and then reference the appropriate Display State in the Drawing.

16. “I want to dimension to the edge of a circle (or hole, radius, etc.) instead of to the center. How can I do that?"

With the Smart Dimension function active, hold down your Shift key while selecting the circle. That will place the dimension to the edge (near or far edge, depending on where you clicked) instead of the center. If you already placed the dimension, you don't need to delete it. Just click on it to highlight it and bring up it's PropertyManager, then go to the Leaders tab. Center will be selected by default, but you can change it to either Min or Max, depending on your needs. The screenshot below is from a sketch in a Part, but the same principles work with dimensions in a Drawing.

This assumes that you were referring to placing a dimension with the Smart Dimension function in a Drawing, or in a sketch in a Part or Assembly. If you're using the Measure tool from the Evaluate toolbar and want to measure to the edge of a hole or circle instead of to the center, then click on the Arc/Circle Measurements icon and choose the appropriate setting from the drop-down. Keep in mind that while Center to Center is the default setting, SW will remember your last setting the next time you activate the tool. It won't go back to the default.

17. “I want to place a drawing view with a specific orientation that's not one of the standard views. How can I do that?"

Like most things in SolidWorks, there are several ways this can be done. Probably the simplest starts with orienting the model the way you want the drawing view to be. That can be done a variety of ways, such as starting with one of the standard views and rotating by holding down Ctrl and using the right and left arrow keys on your keyboard, or by Ctrl+selecting two non-parallel surfaces and then the Normal to button from the Standard Views toolbar (which will place the model with the first face selected normal to your screen, and the second surface selected at top). When you have the model oriented the way you want, hit your spacebar. That will bring up the Orientation dialog box. Select the New View icon.

Name your view and save, and the View will be available to use in your Drawing. Select it from the view's PropertyManager.

If your drawing view has the correct face normal to the screen, but you need to rotate it, you don't need to create a new view. Just click on the drawing view to highlight it, then click on the Rotate View icon in your heads-up toolbar (see below). That will allow you to enter a value for how much you want to rotate it. It will rotate counter-clockwise, so if you want it rotated 90° clockwise you'll need to enter -90°. By the way, I occasionally have a body that comes into the drawing at an odd angle because that's how it's oriented in the model. When that happens, and I want it horizontal or vertical, I place a sketched line in the view, make it horizontal or vertical, then use the Smart Dimension or Measure tool to determine the angle between it and a model edge. That's a big help with knowing what value to enter for Rotating the view. Delete the line after determining the value.

An option I recently (2017-06-15) learned about for rotating a view is to select an edge of a drawing view, go to Tools > Align Drawing View, and select "Horizontal Edge", "Vertical Edge", etc., but you may or may not get the results you want. See the comments on page 7 of this Discussion.

Still another option for drawing views of Parts is to go ahead and insert a view, then right-click on it and choose Drawing Views > Relative View.

That will take you to the model where you can choose which faces (or Planes) you want front and right. If this is a multi-body part you will also have an option to choose which body or bodies you want included in the view. When you click OK in your model it will place a new drawing view oriented according to your selections. You can now delete the original view if it's not needed. Relative View was one method commonly used for showing selected bodies before the Select Bodies... button shown in #15 above was added, but I don't believe I've used this method since then. Once you've clicked Okay you can't go back and edit your selections, which is one big reason I don't like to use it. I described it here because it's an option for a drawing view orientation without the need to create a new view in the Part file. This also might be a good option if you're in a multiple user environment, because if someone updates the model's standard views it won't affect drawing views that were inserted using this method.

18. “I have customized my SolidWorks settings (active toolbars, keyboard shortcuts, System Options, etc.) from the default settings. Is there a way to save these, or share them with someone else?"

Yes, the Copy Settings Wizard will do that. It will let you save a file with all your toolbars, menu selections, other workspace settings, and also your settings at Tools > Options > System Options. You can then go back to the Copy Settings Wizard to load these settings when needed. While it's perfectly fine to save this file to your hard drive, I'd suggest keeping a backup on a network, flash drive, etc. in case your computer dies, or for when you get a new one. And it doesn't automatically update, so to keep it current you need to save a file every time you make changes.

There are several ways to get to it. If you have SW open, you can go to Tools > Save/Restore Settings...

...or go to the SolidWorks Resources tab on the Task Pane and choose Copy Settings Wizard in the SolidWorks Tools section.

If you don't have SW open you can get to it by going to Start > All Programs > SolidWorks > SolidWorks Tools > Copy Settings Wizard.

19. “Can a cut or Hole Wizard feature created in an Assembly show in the Part files?"

Yes. Check the box shown below, then choose All components or Selected components. If you chooseSelected components you will likely need to un-check the box for Auto-select, and then choose which Part files you want the feature to propagate to. Also keep in mind that if you choose "All components" it will affect components that are added after the feature. I found this out the hard way (it took me longer than it should have to figure out why my washer didn't look right after it was mated to the hole).

20. “I deleted a row from my BOM, and now there is a skip in my balloon numbers. How can I fix that?"

Ctrl+select (or Shift+select) each row below the skipped number and drag them above the skipped row. That will fix the issue, but if your assembly is edited, and new parts added, they will be placed at the bottom of your BOM and the skip in numbers will be back until you drag the new row up.

In the future I'd recommend moving the row to the bottom of the BOM first, and then Hide it instead of deleting it so you can get it back if you change your mind. An even better option is to open the assembly, find the component in the tree, click on the Component Properties icon...

...and select "Exclude from bill of materials" at the lower right corner of the Component Properties dialog box.

21. “I'm trying to create a Linear (or Circular) Pattern in my part but it doesn't work right. What's wrong?"

If you are trying to pattern a feature (such as an Extruded Cut) and having problems, try selecting "Geometry Pattern" under Options. If you're trying to pattern a body, be aware that "Features and Faces" will be selected by default. You will get better results if you de-select that box and select Bodies (purple arrow) instead, then select the body or bodies to pattern. Failing to do that is a common mistake.

If you've already created the pattern, and are using SW2014 or earlier, you'll need to delete this pattern and create a new one, this time choosing Bodies instead. Beginning with SW2015 you can edit the feature and make that change (you'll need to un-check the Features and Faces box and clear it's selection box, then proceed withBodies). This is also true for Mirroring bodies.

If that's not the problem, and you're working with a multi-body Part and only want to pattern a single body, check to be sure this body hasn't been merged with another body or bodies.

Speaking of patterns, I never use patterns in sketches. I have found that it works much better to create a single feature or body with the sketch, then pattern it. There may be situations where this isn't true, but I have never run into one. Mirroring sketch elements, on the other hand, usually works pretty well, and I do it often.

22. “How can I create an arrow without text in a drawing?"

There are at least two methods. The first is Insert > Annotations > Multi-jog Leader. Click on the drawing to place the end of the first arrow, then move your cursor to where you want the other end and double-click to place it and exit the command. Next right-click on one end to choose straight line (or whatever you want) instead of the arrow head.

I just recently learned of this method, and I've had a little trouble with getting the Leader to belong to a drawing view, but that may just be one of those little tricks that SolidWorks does just for me (it wouldn't be the first time that happened). I even had a case where I would move the drawing view, and one end of the leader would move with it and the other wouldn't. If that happens to you also then I'd suggest another method. Activate the Note command. Place the end of the leader on some geometry of the drawing view you want the leader to belong to (you can drag it away later if needed), and then when the text box appears just hit your Space bar. That will create a leader without a visible text box. This method may be a little quicker (not sure about that), but with the Multi-jog Leader the leader will snap to horizontal or vertical, which can be very helpful.

23. “When I use the Zoom to Fit feature, my model (or drawing sheet) is thrown way off to one side. Why?"

If this is in an Assembly, you likely have a small Part that's a good distance away from the rest of your Assembly. Click-and-drag a box on the apparently blank space to select anything that's out there, then hit the Delete button. Now try Shift+C again to see if that fixed the problem. If that doesn't work check your sketches to see if there's a stray sketch element or dimension out there. These are only a few of the possibilities; there are others (see Thomas and John's comments on page 3 of this Discussion), but something is almost certainly out there.

If it's in a drawing you may have a small sketch element that's causing the problem. Try the same method. If this is a drawing view of an Assembly, with some components hidden, the drawing view outline will still encompass the whole model. Do a Cropped View around the visible components. That should fix it. If you're using SW2015 or later you can use the Zoom to Sheet function (SolidWorks Help - Zoom to Sheet; thank you Kelvin, I had forgotten about that), which will ignore the drawing view boundary.

24. “I used the Mirror Component function in my Assembly, but the new component is turned wrong. How can I fix it?"

Edit the feature and click on the blue arrow at the top of the feature's PropertyManager.

That will take you to the second page of the PM, where you can select which orientation you want. If you've mirrored multiple components you'll need to click on each one in the Orient Components box and fix each one.

25. “My drawing dimensions are showing the wrong standard (millimeters instead of inches, etc). How do I change this?"

For a quick change you can go to the bottom of your monitor and make the change with the flyout.

This flyout is a fairly recent enhancement. If you're using an earlier version that doesn't have it, go to Tools > Options > Document Properties > Units. If you do have the flyout you may need to go there anyway to refine some settings. Below is a screenshot of the settings for my drawing template. Dimensions display as inches because "IPS (inch, pound, second)" is selected, and they're rounded to the nearest 1/16 because I entered 16 in the Fractions column. You can enter 8, 32, or whatever is appropriate for your drawing. When I took the screenshot I had clicked on the cell in the More column to show the fly-out. If you have similar settings, but an occasional dimension displays as decimal instead of fraction, then it's because you don't have "Round to Nearest Fraction" selected.

If you want your dimensions to show as decimals instead of fractions, then click on the drop-down arrow in the Decimals cell and make the appropriate selection for the number of digits you want to display. (I almost always choose 4 digits because it bothers me to no end to see 1/16, 5/16, etc. rounded off, but that's just a personal quirk.)

If on the other hand your drawing is displaying inches and you want millimeters, change the setting to "MMGS (millimeter, gram, second)" at top and choose the appropriate number of decimals you want to show from the Decimals column. If you want your dimensions rounded to the nearest millimeter you'd select "None" from the drop-down. If you want something that's not a standard Unit system, such as feet and inches, then select "Custom" and make your selection from the drop-down in the Unit column.

By default, even if you have something other than "None" selected in the Decimals column and a dimension is an even millimeter, (inch, etc.), then the zeros past the decimal point won't show. If you want them to show, then go to Tools > Options > Document Properties and select "Show" from the drop-down shown below.

If this change is something you want for future use, be sure to save it in your drawing template.

In number 2, you could also mention the need to use the File Locations option to store the changed template in a non-installation folder to prevent it being overwritten by an update or upgrade. Also to use the Default Templates option.

5. “I saved a Toolbox part to a new name and made some changes. I used it IN an assembly and saved the assembly, then when I opened the assembly it’s been replaced by another Toolbox part. What happened?”